## General Mechanical

Topics relate to Mechanical Enterprise, Motion, Additive Print and more

#### Honeycomb acting too stiff

• Basil Tschudi
Subscriber

Hi everyone
I'm currently modelling a honeycomb insertsystem for my bachelors thesis. However compared to the real world tests the simulation is acting waaaaay too stiff. I modelled the honeycomb as a solid and adjusted the material propreties accordingly. However i suspect that the stiff behaviour is resulting due to the surface which is bonded to the facesheet being too big (because it's modelled as a solid). So i guess I'd have to reduce the surface of the honeycomb. Some sort of trimming. I have no idea how to do that in Ansys though. I do have the factor that I.d need to implement.
Any ideas?

• Nanda Veralla
Ansys Employee

Hello Basil,

Looks like you have a bolt in the center that is keeping the assembly together. I suspect the higher stiffness is because of the contacts you’ve given. Here are the contact definitons you should give:

1. Frictional between U shaped bottom face and flat sheet’s top face.
2. Frcitional between bolt head’s bottom face and top face of U shaped solid.
3. Frictional between Nut’s top face and sheet’s bottom face.
4. Frictional between Bolt’s circular face and sheet’s hole where bolt sits.
5. Bonded should be only given between Nut and Bolt.

If you have any pretension defined, make sure the axis of pretension doesn’t coincide with defined bonded contact region.

Definition Settings (ansys.com)

Preloaded Bolted Joint Analysis | Ansys Innovation Courses

Regards,

Nanda.

Guidelines for Posting on Ansys Learning Forum

How to access ANSYS help links

• Basil Tschudi
Subscriber

Hi Nanda

The Bolt is only modelled very crudely as it's not the main focus of the simulation. the force is indirectly intoduced through a backingplate at the bottom side of the sandwich. I put a picture of the crosssection of the insertsystem at the bottom.

Face sheets are yellow, core is red, potting compound is blue, insert and U-shaped mount are grey and the backing plate is black/dark grey. The hole i the middle of the insert is not threaded and the force is introduced perpendicular to the faceshets.

• peteroznewman
Subscriber

I suggest you rework the geometry so you can mesh the facesheets with shell elements and eliminate bonded contact between the facesheets and the core solid. You do this by using Shared Topology. The benefit of using shell elements is that the thickness of the facesheet is easily adjusted to help match experimental data on the bending stiffness of the sandwich. The shell elements are given an offset to put the thickness above the nodes on the top surface and below the nodes on the bottom surface.

Prepare the geometry by deleting the facesheet solids. In SpaceClaim, make a New Component, select the face of the core and type Ctrl-C and Ctrl-V to copy the face and paste a surface into Component1. On the Workbench tab, you will click the Share button. That will cause the shell mesh on the surface to share the same nodes as the solid elements on the core solid. It will be best if you mesh the solid core using a Multizone or Sweep method to get Hex-shaped elements. If you use sweep, set the number of sweep elements to 4 through the thickness of the core. Set the Mesh Element Order to Linear which will reduce the number of nodes in the model and reduce the solution time.

Make another New Component and drag the solid for the potting adhesive (blue) and drop it into Component2. Repeat for the metallic insert and the bottom plate.

Create additional surfaces (or planes) so you can use them to cut all bodies along the red lines shown below to make a sweep mesh possible. When you are done, use the Share button on all components to connect all the separate bodies using the mesh.

The lower metal plate could also be converted to a Midsurface and meshed with shell elements. It can make frictional contact with the facesheet shell elements, you just need to put the offset (facesheet thickness + 1/2 plate thickness) into the contact definition.

• Basil Tschudi
Subscriber

The facesheets are already shell elements as they are modeled in ACP(pre) and then imported into the model as shell elements.

• Basil Tschudi
Subscriber

Also I reckon it's important to say that the node does work and give a solid solution with absolutely plausible deformations and stress distributions. It's just too stiff🤷🏽‍♂️

• peteroznewman
Subscriber

Did you create an orthotropic material for the honeycomb core?  Do the Global coordinates align with the relevant axes in the othrotropic material definition?  This discussion has an example of an orthotropic material model for a honeycomb core.

You can adjust the shear modulus value to match the experimental data.  What do you have for experimental data?  How did you measure the stiffness of your Ansys model?

• Basil Tschudi
Subscriber

Yes and yes!
I've been working on it the past few hours and by now I feel like the shear moduli are off.

I'm comparing the ansys model to the real tests I performed with the identical models. For the same force the real world model had a displacement of around 10 mm whereas the anys model computes arounf 2.5mm.

• Basil Tschudi
Subscriber

• peteroznewman
Subscriber

Where did you get the initial values for the shear modulus?  Was it from a manufacturers data sheet?

I assume the tet elements are quadratic. Two layers of quadratic elements is a minimum. Linear tet elements would be overly stiff.

• Basil Tschudi
Subscriber

I dont remember exactly i think it's from a paper about something like this not from the manufacturer. However i guess they should be plausible...

yes they are quadratic and small enough

• peteroznewman
Subscriber

Please describe the supports on the FEM and the physical sample. Please describe what equipment is used to measure the stiffness of the physical sample.

Often the idealized nature of the supports in the FEM adds stiffness that is not  representative of the physical sample.

How is the force and displacement being measured? Is the sample in an Instron Tensile Testing machine?  Do you have photos you can show?

• Basil Tschudi
Subscriber

This probably explains most. The panel is vlamped between two steel plates and four bolts one on each corner. Force and displacement are measured by the machine.

• Basil Tschudi
Subscriber

The supports are: fixed displacement in z for the surfaces representing the steel frames on the top and bottom of the panel (i knkw they should be compression only but that somehow does not work on the ACP things) and fixed displacement in x and y for the bolt holes

• peteroznewman
Subscriber

I suggest you add the top steel plate as a midsurface to your model and put frictional contact between it and the top surface of your sandwich. I would also add four beam elements from the hole centers in the steel plate down to where the threads enter the bottom plate. Use a Fixed Support at the bottom of the four beam elements.  Use a Fixed Joint to connect the top of the beam to the hole in the steel plate. This will allow your sandwich to bow the top steel plate up along the sides and allow the bolts to bend a little, which will more accurately reflect deformations in the test fixure and sandwich. The added flexiblity in your model will reduce the calculated stiffness.